I recently stopped by and was told that the CNC was dead, or at least not working right, so I took it upon myself to dismantle the motor and spindle, re-oil everything, fix the belt tension, etc. It mills aluminum just fine now, as long as you don't try to take too heavy of a cut. I'm going to start working on a PCB mount system as well. - cole

I recently stopped by and was told that the CNC was dead, or at least not working right, so I took it upon myself to dismantle the motor and spindle, re-oil everything, fix the belt tension, etc. It mills aluminum just fine now, as long as you don't try to take too heavy of a cut. I'm going to start working on a PCB mount system as well. - cole

+

+

Guys, I'd like to start using MaxNC for making PCB now, but I didn't see any PCB mount system around here. Are you guys still hanging out here? [[User:Azureviolin | Hao Zhang]] 16:09, 9 June 2012

USE EYE PROTECTION unless you like tweezering pieces of shattered carbide mill tools out of them

Though we have implemented basic safety shutoffs, we should be watching it all the time. It will very happily mill through itself without stopping.

If it appears to be getting out of hand, the F1 key should toggle Emergency Stop in the software. This will power down the spindle and stop it where it is immediately.

If it REALLY IS getting out of hand, turn the power switch off (the one on the side of the control box). Note however that after doing this you'll probably need to restart the software because it will be out of sync with the controller (it gets out of sync).

The resulting binary should run and give you a UI on your system. There's actually nothing machine-specific that you need at this point: your UI will look pretty much exactly what we have now. Select the "axis.ini" config file.

You should now just be able to:

open one of the sample gcode files

power the machine 'on' (unset emergency stop [red X], and set power [orange square] buttons)

'home' the various axes (must home all axes, use radio buttons to select)

'run' the gcode. (blue "play" triangle)

For most of the configurations there is a smaller window w/ an inverted cone representing the spindle (this is the default view). This will show the progress of your milling run. You can change the view and pan/zoom/tilt with the mouse.

For a sanity check, try simulating a run of the NB logo gcode from Identity

Text /TrueType

DXF/QCAD

DXF is a standard file format used by many CAD programs (as well as exportable from inkscape and Adobe Illustrator). It's a good choice, especially as gcode export from Inkscape seems to be buggy.

QCAD is an open-source 2d CAD program. Linux users can apt-get qcad, there is open-source executable for Windows as well (but it's hard to find as Ribbonsoft took it closed-source (wtf?) and most searches end up at their page.) QCAD is very solid and a great place to start with CAD, especially if you can't afford/don't need Autodesk/Solidworks.

The scale feature in QCAD is counterintuitive at first. To scale your object, select all, then select Modify -> Scale. Click the right arrow on the bottom of the toolbar on the left side. It will then ask for a reference point, click on the lower left corner of your image. It will then ask for the scale factor and will scale your object.

Open your dxf file from File->Read DXF. It sometimes barfs on DXF exported from Inkscape (works fine for me), but is fine with QCAD, so a workaround is to load the Inkscape dxf in QCAD and save it from QCAD (it's also easy to scale and rotate if necessary).

I am still working through the various dxf2gcode options but setting "infeed depth" to the same value as "mill depth" gives you a one-pass toolpath (otherwise it seems to do it in two passes.)

Coordinate units are kind of a crapshoot and don't make much sense right now.

Note that it may be doing a lot of math without benefit of the numpy library so it can be SLOW. It has no progress indication, and doesn't redraw the screen, so it may look like it crashed. Sometimes it actually does. But be patient!

Sometimes it gives the error "Failure reading like stopped at line X. Please check/correct line in dxf file." If X is the number of lines in your DXF, don't worry, it read the whole thing.

By default it lifts the tool up unnecessarily high, you can improve cutting speed by setting the Z retraction area and Z safety margin to a lower number than the default of 15.

EagleCAD

Cadsoft EagleCAD is a schematic editor and PCB layout tool. It's not open source, but there's a
free version that is very decent and limited only to the size of board you can lay out.

To generate GCode from your Eagle layout, get the scripts from http://www.pcbgcode.org/. These do "Isolation routing," that is, they will generate GCode to mill away copper outside the traces you laid out on a copper-covered PCB (as well as drill it).

I've added MAXCNC mill-specific commands to the pcbgcode config stuff, including setting the spindle speed to maximum and turning on the motor. (Config file is /home/nb/eagle-5.6.0/ulp/gcode-defaults.h on the mill PC).

To start, create a layout in Eaglecad. To work best, use one layer (which can make routing a pain), and use a minimum trace size of 0.012 inches. Make sure you do a DRC check with 10 mil isolation spacing (thouugh I have found it misses trace-pad distances).

From the Eagle command line,

run pcb-gcode-setup

This creates several gcode .ngc file in the same directory as your eagle .brd file. They have suffixes like
"top" "bot" and "d" for top copper, bottom copper, and drill. Run AXIS2 and load the appropriate file. Look CAREFULLY at the tool path. Does it really isolate everything you want it to? If not, you may have to increase spacing and re-run. Check especially places of small pitch and tight clearances, especially between traces and pads.

Milling the copper is a tradeoff between quality and speed. At fast speeds, the copper tends to get rough at the milled edges. Slow speed rates help a lot but can lead to impractically long milling times.

2.5 ips gives beautiful results, but a good compromise is something like 5 - 8 ips (set in the pcb-gecode setup). If you look at File->properties in the EMC2-Axis tool it will give you a rough idea of the milling time.

Setting the Z home at precisely zero (at the board surface) is very important, because we are working at depths of hundredths of an inch. After several attempts I don't think you can do this well with just the manual jog, and risk breaking the tool. Here's what I did that worked:

Raise the head so you can put the tool in the collet. Put it in as far as you can.

Tighten gently, only enough to keep from falling out.

Drop the head to about 1/4 an inch above the workpiece. Don't touch!

Loosen the mill tool in the collet

GENTLY let the mill tool drop to touch the workpiece surface

finger-tighten the collet -- tightly!

Home the Z axis VERY IMPORTANT DON'T FORGET!!

Raise the head and wrench-tighten the collet

I think the default Z Down dimension of -0.01 may be too much given that 1-oz copper is supposed to be only 1.4 mils thick (0.0014 inches). I've had good results with -0.008; .0.005 led to problems because I think the PCB I used was not perfectly flat at at some places this depth did not hit "bottom." With further experiments this may be because the clamps are compressing the PCB: at least it seemed to work fine more than 1/2 inch away from them.

Drilling vias

For through-hole components, you'll need to drill vias. Doing this is a multi-step, involved process. Because etching is sensitive to the trueness/truing of your board's surface, you only want to etch the board when it's mated directly to a metal block, but you need a plastic sacrificial stop for drilling. So, etch as normal, then add two registration marks to the top of the board. Unmount it, add the plastic backing, change tools, remount, and rezero, respecting the registration. From there, you can run the drill program after suitable modification (you need to manually comment out all M06/tool change commands).

Generating the drill file:

Settings specific to drilling:

Machine:

Tool Change: you can't actually change tools at the moment, so this is just to expedite your cutting process, and stay within the limits of the mill

X: 0.0

Y: 0.0

Z: 0.2

Drill depth: Measure your board with calipers, then add 10mil for good measure (I used -0.100" for the single-sided board I did yesterday)

GCode Options:

Ensure "Do tool change with zero step" is UNCHECKED. If this is checked, EMC hangs. No, really, you don't want to deal with this problem. It's awful close to "EMC hangs, you have to hard kill it, and then rezero the whole setup."

Once you've got the GCode files for etching and drilling generated, you need to tweak the drill file. As it's currently configured, our milling rig doesn't handle tool changes well (the CNC doesn't support automatic tool change, but the EMC software thinks it does, so the whole setup gets Very Unhappy when it runs into these commands). To remove these, open your drill ngc/tap file in a Text Editor Of Your Choice, and comment out all lines containing the tool change command M06. In GCode, comments are parenthesized lines, and they cannot be nested.

Open your drill file in EMC and make sure it looks sane. There will be a bunch of tool change steps, where it runs itself back to (0,0,0.2), then goes back to work. This is the tool change position specified above; you may want adjust the point to be closer to the centroid of your drill pads, to shave off a minute or two.

After your etch file looks good, and your drill files look reasonably good, go ahead and set up for etching as above. When etching is completed, don't take the board out! We need to add registration marks for the remounting. Manually walk the head down to (0,0,0.5). Once you're there, turn on the spindle, and gently lower the head til it just bites the copper. Personally, I went to (0,0,-0.008), which is the depth used for etching. Leave the spindle on, and raise the head back to (0,0,0.5). You can turn the spindle off if you'd like, then slew over to (1,1,0.5). Once there, turn the spindle back on, and go down to (1,1,-0.008) to make the second registration mark. Raise the head out of the board, then turn off the spindle. I'd also recommend slewing back to (0,0) at this point, to make re-registration easier.

Next, load up the drill file in EMC. You should still have the outline of the paths the head just etched on the display, with the drill file overlaid. This is a good chance to sanity check the line-up of things, etc. Once that looks right, move to adding a plastic backstop and re-rigging the board.

With those two registration marks in place, you can re-rig the board with a sacrificial plastic backstop underneath of it. There's a few of these in the document trays next to the mill. Change out to your PCB drill-end, re-zero as for etching, and ensure you have good registration (make sure the drill-end is sitting on the 0,0 mark when you insert it, raise to (0,0,0.1), and slew to (1,1,0.01) to eyeball the match up. If you want to be totally certain, you can turn the spindle on and just bite the board, but, in doing so, you're likely to obliterate your registration mark, so I'd advise against that.

Make sure you're happy with everything, and, assuming you are, hit Run. Keep an eye on things and be ready to hit the kill switch (if babysitting feels tedious, just imagine yourself doing all these holes on the drill press, and then try not to hug your newfound robot slave/friend). -- User:Jbm 2010-05-07 13:20; a big thank-you to User:jtfoote for all his help in familiarizing me with the setup.

Tooling

Cutting fiberglass (PCB) will eventually destroy any kind of steel cutting tool. The glass in the resin matrix is much harder than steel. You need carbide tooling. Note that carbide is too brittle for most metals and will just snap.

Search for "small parts inc" on amazon.com. They have reasonable prices and reasonable shipping for endmills. (You can also search for endmills) I believe we have a 1/4" and 1/8" collet for the mill, so you're looking for tools with a 1/4" or 1/8" shank. I mostly bought HSS for cutting plastic, but I have some harder ones with exotic coatings for aluminum and brass. --lamont

User:seph was hacking on one. Some notes from him are at http://www.directionless.org/tmp/maxnc/
There's a pinout, and an emc2 config. He also recommends thinking about eventually upgrading a lot of the components. Seph's work is what I (mikew) based the current functional HAL and INI files on.

Workpiece holders are small threaded rods with metal "clips" that are designed to hold the workpiece firmly to the bed. They should not be over-tightened, as it can cause workpiece distortion.

Backing material is a piece of scrap material used between the bed and workpiece. It's important to use backing material to protect the bed.

Limit switches are located at the end of each axis. These act as safeties in case the milling machine reaches the end of its travel. Note: if you're milling and manage to trip a limit switch, the mill shuts off, in which case you'll need to redo your work. Be diligent.

The X axis runs side to side; e.g. the "width" of the bed.

The Y axis runs forward and back; e.g. the "depth" of the bed.

The Z axis runs up and down; e.g. the space between the bed and collet.

Affixing the workpiece to the mill

Use a piece of aluminum stock between the PCB and the bed.

Use adjustable wrenches to cinch down the workpiece holders to the PCB. You only want the bolts to be finger-tight; the fiberglass substrate can actually be compressed if too much pressure is used, causing distortions in the milled part. Do not use pliers.

The collet faces upwards (like the tip of a rocket) into the spindle.

Keep the plastic guard attached to the milling bit. Place the bit into the collet, and bolt the collet into the spindle.

Zeroing the machine

Note: In the MaxNC control program, it's important to zero the mill - to set it to 0,0,0 - before routing a board. Occasionally, the milling machine will not home to 0,0,0 in the MaxNC control program. To fix this, go to Machine > Zero Coordinate System > P1 G54.

In AXIS' Manual Control tab, adjust the X, Y, and Z axis feed controls until the tool is at the upper right corner of the circuit board.

Chuck the bit, finger-tight.

It is critical to zero the Z axis correctly. The idea is to drop the bit down onto the surface of the copper, with zero force, and then zero the axis. Use the manual controls to drop the bit, step by step, until it is about 1/4" above the surface of the PCB.

Loosen the collet so that the bit drops onto the board. Tighten the collet.

Immediately zero the Z axis.

Milling

Controls for starting / stepping / stopping milling operations are located in AXIS' top toolbar.

At this point, all of the axes should be zeroed.

Click the Go button in the toolbar to start milling.

Upgrade

I'd like to upgrade the maxnc. Right now its a bit sloppy. I want to (1) fix it up, (2) make a locating system for two-sided PCBs, (3) make a sweet document with tons of pictures so its easy. -moo

Hey moo, who are you?
The mill seems plenty accurate for our purposes, are you finding it isn't? (though a pcb jig would be sweet).
I think someone bent the X spindle through misuse, if we fix anything let's fix that... Jtfoote 05:37, 13 May 2010 (UTC)

I recently stopped by and was told that the CNC was dead, or at least not working right, so I took it upon myself to dismantle the motor and spindle, re-oil everything, fix the belt tension, etc. It mills aluminum just fine now, as long as you don't try to take too heavy of a cut. I'm going to start working on a PCB mount system as well. - cole

Guys, I'd like to start using MaxNC for making PCB now, but I didn't see any PCB mount system around here. Are you guys still hanging out here? Hao Zhang 16:09, 9 June 2012